Monday, September 23, 2013

Ruminating Rigid Flex - Part 4


It’s easy to look at the problems of layer stack design, parts placement, and cutouts and think we’ve got the issues down. But remember in my first blog in this series how flex circuits have some gnarly material quirks. Quirks ranging from relatively high z-axis expansion coefficients of adhesives, to the lower adhesion of copper to PI substrate and coverlay, to copper’s work hardening and fatigue. These can be compensated for largely by following some Dos and Don’ts.

Do Keep Flex Flexible

This may seem obvious, but it’s worth saying. Decide just how much flex is needed up front. What I mean is; if your flex-circuit sections are only going to be folded during assembly and then left in a fixed position - such as in a handheld ultrasound device - then you are a lot freer in the number of layers, the type of copper (RA or ED) and so on you can use. On the other hand, if your flex-circuit sections are going to be continually moving, bending or rolling, then you should reduce the number of layers for each sub-stack of flex, and choose adhesiveless substrates.

Then, you can use the equations found in IPC-2223B (Eq. 1 for single-sided, Eq. 2 for double, etc.) to determine what is your minimum allowable bending radius for the flex section, based on your allowed deformation of copper and the characteristics of the other materials.

This example equation is for single-sided flex. You need to choose EB based on the target application, with 16% for single-crease installation of RA copper, 10% “flex-to-install” and 0.3% for “dynamic” flex designs (Source: IPC-2223B, 2008 Here, dynamic means continuous flex and roll during use of the product, such as a TFT panel connection on a mobile DVD player.

Don’t Bend at Corners

It is generally best to keep copper traces at right-angles to a flex-circuit bend. However there are some design situations where it’s unavoidable. In those cases keep the track work as gently curving as possible, and as the mechanical product design dictates, you could use conical radius bends.

Figure 1: Preferred bend locations.

Do Use Curved Traces

Also referring to figure 1 above, it’s best to avoid abrupt hard right-angle trackwork, and even better than using 45° hard corners, route the tracks with arc corner modes. This reduces stresses in the copper during bending.

Don’t Abruptly Change Widths

Whenever you have a track entering a pad, particularly when there is an aligned row of them as in a flex-circuit terminator (shown below), this will form a weak spot where the copper will be fatigued over time. Unless there is going to be stiffener applied or a one-time crease, it’s advisable to taper down from the pads (hint: teardrop the pads and vias in the flex circuit!)

Figure 2: Trace width change and pad entries can cause weak spots.

Do use Hatched Polygons

Sometimes it’s necessary to carry a power or ground plane on a flex circuit. Using solid copper pours is okay, as long as you don’t mind significantly reduced flexibility, and possible buckling of the copper under tight-radius bends. Generally it’s best to use hatched polygons to retain a high level of flexibility.

While thinking about this one, it also occurred to me that a normal hatched polygon still has heavily biased copper stresses in 0°, 90°, and 45° angle directions, due to alignment of hatch traces and ‘X’es. A more statistically optimal hatch pattern would be hexagonal. This could be done using a negative plane layer and an array of hexagonal anti-pads, but I found it fast enough to build the hatch below with cut-and-past.

Figure 3: Using hexagonal hatched polygons can spread the tension biases evenly among three angles.

Do Add Support for Pads

Copper on a flex circuit is more likely to detach from a polyimide substrate, due to the repeated stresses involved in bending as well as the lower adhesion (relative to FR-4). It is especially important therefore to provide support for exposed copper. Vias are inherently supported because the through-hole plating offers a suitable mechanical anchor from one flex layer to another. For this reason (as well as z-axis expansion) many fabricators will recommend additional through-hole plating of up to 1.5 mils for rigid-flex and flex circuits. Surface mount pads and non-plated-through pads are referred to as unsupported, and need additional measures to prevent detachment.

Figure 4: Supporting through-hole pads in flex with plating, anchoring stubs, and reduced coverlay access openings.

Referring to figure 4, the second option is good for adhesive coverlay and the third for adhesiveless. Coverlays attached with adhesive will exhibit “squeeze out” of the adhesive, so the pad land and the access opening must be large enough to allow for this while providing a good solder fillet.

SMT component pads are among the most vulnerable, especially as the flex circuit may bend under the component’s rigid pin and solder fillet. Figures 5 and 6 show how using the coverlay “mask” openings to anchor pads one 2 sides will solve the problem. To do this while still allowing the right amount of solder the pads have to be somewhat larger than typical rigid-board footprints would have. This is compared in figure 6, with the bottom SMD footprint used for flex mounted components. This obviously reduces the density of flex circuit component mounting, but by nature flex circuits cannot be very dense compared with rigid.

Figure 5: Coverlay openings for an SOW package showing anchoring at each end of each pad.

Figure 6: Adjusting the pad sizes and “mask” opening for coverlay. The top land pattern is for a nominal 0603 size chip component, whereas the bottom is modified for coverlay anchoring.

Double-Sided Flex

For dynamic double-sided flex circuits, try to avoid laying traces over each other on the same direction (figure 7). Rather stagger them so the tensions are more evenly distributed between copper layers (figure 8).

Figure 7: Adjacent-layer copper traces are not recommended.

Figure 8: Staggered adjacent-layer traces are preferred.

This is by no means a complete set, but You should now have a few good tips on how to design flex circuits to give the best yield and highest reliability for the product - but be aware of the tradeoffs between cost, performance and reliability.

In my next blog, I’ll be wanting to whet your rigid-flex appetites, by considering a few example applications of this technology, and hopefully some novel ideas will arise as a result.


Wednesday, September 18, 2013

Ruminating Rigid Flex - Part 3

Fab documentation for flex circuits and rigid-flex boards.

In the last blog on rigid-flex PCBs, I talked about the fabrication processes typically used by board houses. It's important to understand the steps required to build up a rigid-flex or flex circuit PCB because it has a big effect on how you need to design the board. And it also affects what needs to be included in your fabrication data set to send the design to successful fabrication. If you haven't read parts 1 and 2 of this blog, go read them here and here before continuing on.


Let's talk about documentation then. This is essentially where we tell the fabricator what we want, and it's probably the most likely part of the process where errors or misunderstandings can make costly delays happen. Fortunately there are standards we can reference to make sure we are communicating clearly to the fabricator, in particular IPC-2223B (which I am referencing in writing this).

It could boil down to a few golden rules:

  • Make sure your fabricator is capable of building your rigid-flex design.
  • Make sure they collaborate with you on designing your layer stack to fit their particular processes.

·         Use IPC-2223 as your point of reference for design, making sure the fabricator uses the same & related IPC standards - so they are using the same terminology as you.

  • Involve them as early as possible in the process.

Output Data Set

In interviewing a handful of rigid-flex capable board houses locally, we found that many designers still present gerber files to the board house. However ODB++ v7.0 or later is preferred, since it has specific layer types added to the job matrix that enable clear flex-circuit documentation for GenFlex® and similar CAM tools. A subset of the data included is shown in table 1.

Table 1: Subset of Layer Types in ODB++ (v7.0 and later) used for GenFlex

(Source: ODB++ v7.0 Specification)

Layer Type

Base Type




Clearances of a coverlay layer



Clearances of a covercoat layer



Pattern for die-punching of the flex circuit



Shapes and locations of stiffeners to be adhered

Bend Area


Labelling of areas that will be bent while in use



Pressure Sensitive Adhesive shapes and locations



An area definition (Rigid, Flex, or arbitrary)

Exposed Area


An exposed area of an inner layer and its associated coverlay (could also be used for embedded components)

Signal Flex


A signal layer for a flex circuit

Power Ground Flex


A power of ground layer for a flex circuit

Mixed Flex


Mixed layer for a flex circuit

Plating mask


A mask for defining which areas within a layer should be masked off from plating process

Immersion Mask


A mask for defining which areas within a layer should be masked off for immersion gold

There are some issues we face if using gerber for the output data set, or earlier versions of ODB++. Namely, the fabricator will need separate route tool paths and die cut patterns for each rigid and flex circuit section in the layer stack. Effectively, mechanical layer films would need to be produced to show where voids need to be in the rigid areas, and more to show where coverlay or covercoat will be on the exposed flex circuit areas. The coverlay or covercoat also has to be considered a mask for component pads for those components that may be mounted on flex circuit areas.

In addition, careful attention needs to be paid to layer pairs for drilling and through-hole plating, because blind vias from a rigid surface layer down to an opposing flex-circuit layer will have to be back-drilled and add significant cost and lower yield to the fab process.

As a designer, the question is really then, how can I define these areas, layers and stacks?

Define the stack by area using a table

The most important documentation you can provide your fabricator is arguably the layer stack design. Along with this, if you're doing rigid-flex, you have to provide different stacks for different areas, and somehow mark those very clearly. A simple way to do this is make a copy of your board outline on a mechanical layer, and lay down a layer stack table or diagram with a pattern-fill legend for the regions containing the different layer stacks. An example of this is shown in figure 1.

Figure 1: An example of a stack diagram showing fill patterns for rigid and flex circuit areas.

In this example, I used the matching fill patterns for different stack areas to indicate which stackup layers are included in the Flexible part or the Rigid part. You can see here the layer item I named "Dielectric 1" is actually an FR-4 core, which could alternatively be considered a stiffener.

This poses a new problem, in that you also have to define in 2D space where bends and folds can be, and where you will allow components and other critical objects to cross the boundaries of rigid and flexible sections. I will discuss this a little more later on.

Conveying the PCB design intent

We all know a picture is worth a thousand words. If you can generate a 3D image showing flexible and rigid areas this will help the fabricator understand your intent more clearly. Many people do this currently with the MCAD software, after having imported the STEP model from the PCB design. Figure 2 is an example of this concept.

Figure 2: Bending up the mechanical model to show design intent.

This of course can have the added benefit of detecting flex to flex and flex to rigid interferences ahead of epic failure.

Parts Placement

You can see also from the image above, that rigid-flex designs imply that components might exist in layers other than top and bottom. This is a bit tricky in the PCB design software, because normally components must exist on top or bottom. So we need some ability to place components on inner layers.

Interestingly, Altium Designer has always supported pad objects on any layer, so this is not impossible. There's also an implication that silkscreen could exist on flex layers as well. This is not a problem, since coverlay material can adhere well to the silkscreen ink. The trick is more to make sure there's adequate contrast for the color of ink chosen against the coverlay material. Also, resolution is affected since the ink has to traverse a small gap beyond the screen to land on the flex circuit coverlay. Again, this is something that needs to be discussed with the fabricator to determine what's possible and economical.

Side note: If you're going to the effort of drawing the regions of the PCB which are exposed flex layers, and placing components on those regions, this also makes a reasonable method for placing embedded components into cutout regions of the board. You need to generate a set of very clear documents that show where the cutouts are and in which sections of the layer stack they apply. This is going to be limited depending on the fabricators methods - either back-drilling or multiple laminated stack-ups can be used. So communicating your intent and minimizing the number of separate cutout stack sections is important. It's best to completely avoid having intersecting cutouts from opposite sides of the board.

Side-note: Defining Flex Cutout

Notice in figure 1 how there are no hard corners, but rather there's a minimum radius to each angle? IPC recommends greater radii than 1.5mm (about 60 mils), to reduce the risk of tearing of the flex circuit at corners. The same goes for slots and slits in the flex - make sure there's a designed-in relief hole at each end of diameter 3mm (⅛") or more. Another example of this is shown below.

Figure 3: Slots, slits and inside corners should have tear-relief holes or tangent curves with minimum 1.5mm radius.

In order to produce reliable rigid-flex based products, there are many considerations relating the fabrication and the end-use of the flex circuit, to the design of the copper pattern. In the next blog I want to discuss several of these do's and don'ts. Look out for it!